CREO 3.0

assignment1.pdf

Home >Engineering homework help >Mechanical Engineering homework help >CREO 3.0

Lesson 6 – Revolves, Rounds, Chamfers, Threads Lesson 6 is made up of 3 parts which will utilize Revolves, Rounds, Chamfers, and Cosmetic Threads.

The revolve tool is similar to an extrusion but with the addition of diameter dimensions and Axis of

Revolutions. These 3 parts will be used in the future so be sure to save them to your working directory!

Axis of Revolution:

When using the Revolve tool the sketch requires an Axis of

Revolution. This is a specific Axis that has been designated to

revolve the sketch about. The closed-loop MUST not cross over

this Axis!

Axis of Revolution: An Axis of Revolution must be created while

in sketch mode for Revolved features. Without one the feature

cannot be dimensioned or completed.

Hold RMB – select Axis of Revolution – LMB to place the Axis. The Axis of Revolution is now set (dark blue color line).

Creating Revolved Diameter Dimensions:

Revolved Sketches will often require the use of the diameter or revolved dimensions that show the

dimension to the opposite side of the part (or the value it will be once revolved.).

While Using the Normal/Dimension Tool:

1) LMB the Axis of Revolution (Select above/below the sketch lines to ensure you are picking the Axis)

2) LMB the point or sketch line to dimension to

3) LMB the Axis of Re olutio agai , a d MMB to pla e the dia eter di e sio .

Part 1 - Clamp Foot

Step 1 – Set your Working Directory and create a New Part alled Clamp_Foot .

Step 2 – Keep the U its i i h l se a d set the material as Steel.

File- Prepare- Model Properties- Material – change – double-click steel.mtl – OK - Close

Step 3 – Adjust the options so that 3 decimal places will be shown in sketcher.

File – Options – Sketcher – set the Number of decimal places for dimensions to 3 – OK- *No * Don’t other sa ing a Configuration File, as you ould need to load it ea h session to be useful.

Step 4 -1 – Create a Revolve using the RIGHT datum as the sketch plane. Sketch the shape below, placed on the Vertical and Horizontal Axis reference lines as shown.

*Tip: Be sure to set the Axis of Revolution and use Revolved Diameter dimensions where shown.

Step 4-2 – Accept the Sketch and ensure the Revolve is set to 360 degrees. If your Revolve is not visible it is because the sketch is missing an AXIS of REVOLUTION. (Placement - Edit to return to sketch mode and

fix the sketch as needed).

Step 5-1- Create the second Revolve to cut out the inside of the part. Sketch on the RIGHT Datum.

Step 5-2 - Place an Axis of Revolution on the Vertical Reference. Sketch the shape using the Line, Center

and Ends Arc, and Delete Segment tools:

Center and Ends Arc tool – LMB to place the center point on the Axis of Revolution – LMB to place the arc start and end points on the Axis as shown - use the Line tool to place the vertical sketch line. Use

the DELETE SEGMENT tool and LMB click to delete the extra line segments.

Step 5-3 – Use the Normal Tool to create the dimensions as shown. Notice that the dimension of the arc is a Diameter (two arrows) instead of the Radius (one arrow). Follow the step below to make a diameter.

Normal Tool - double click LMB on the curve - MMB to place it. A single click provides a Radius.

Step 5-4 – Accept the sketch and set the options for the Revolve to be REMOVE MATERIAL and 360deg, then checkmark to accept the Revolve.

Step 6 – Add a Chamfer to the cut edge of the Revolve 2 using the Chamfer Tool.

Chamfer tool - set the dimension to be .03125 - LMB the edge of Revolve 2 - Checkmark.

Step 7 – Use the ROUND tool to add Rounds with a radius of .03125 to the 4 outside edges.

Round Tool – Set the radius to .03125 – LMB on the four outer edges - Checkmark

Step 8 – Set the display properties of each datum so that we may use them as a Geometric Tolerance and change them to ASME style in our drawing. We must SET each datum them to be a Geometric

Tolerance and also RENAME them to match the handout/key.

LMB select a Datum from the model tree - hold RMB – Properties - press SET (The middle button) – Click the Name Box – Type in a new name according to the list below – OK. Repeat for each Datum.

RIGHT – Rename to B- Press Set - OK

TOP – Rename to C- Press Set - OK

FRONT – Rename to A- Press Set – OK

Step 9- Save your Clamp Foot part and move on to the next part.

Part 2 – Clamp Ball Step 1 – Set your Working Directory and create a New Part alled Clamp_Ball .

Step 2 – Keep the U its i i h l se a d set the material as Nylon.

File- Prepare- Model Properties- Material – change – double-click nylon.mtl – OK -Close

Step 3 – Adjust the options so that 3 decimal places will be shown in sketcher.

File – Options – Sketcher – set the Number of decimal places for dimensions to 3 – OK- *No

Step 4-1 – Create a Revolve using the RIGHT datum as the sketch plane.

Step 4-2 – Create an Axis of Revolution and sketch the closed loop shape shown below using Center and Ends Arc and the Line Tool. Note: The left vertical sketch line must be a single line that starts at the

bottom and finish at the top of the arc, not the center of the arc. Using two lines in place of a single line

requires extra dimensions.

Step 4-3- Use the Normal Tool to create the shown dimensions*. *Due to the complexity of this shape it

may be required to have the dimension values set all at once using Modify with regenerate turned off.

Modify Dimensions: LMB to drag a selection box across over all dimensions – select the Modify Tool – uncheck Regenerate – type in the values for the dimensions accordingly – press OK.

Step 4-4 – Accept the sketch, and set the Revolve option to 360 degrees. Checkmark the Revolve and Refit to Screen and hold MMB to rotate examine your part.

Step 5 – Use the HOLE Tool to create the first hole. Use the options below:

Type: Standard, Diameter = UNC ½ - 13, Depth = .500, with a Countersink

Placement: COAXIAL Hole

Primary – Axis (that was made from the Revolve 1) & the bottom flat surface of the Revolve 1. Tip: You must selct the Axis first and Hold Control to select the second reference.

Shape Tab Options: Adjust the Countersink diameter to .4844, and the thread depth to .375.

Step 6 – Set the display properties of each datum so that we may use them as a Geometric Tolerance and change them to ASME style in our drawing. We must Set each datum them to be a Geometric

Tolerance and also Rename them to match the handout/key.

RIGHT – Rename to B- Press Set - OK

TOP – Rename to C- Press Set - OK

FRONT – Rename to A- Press Set – OK

Step 7 – Add a CHAMFER to the outer edge the flat surface with a dimension of .03125.

Chamfer Tool - value of .03125 – LMB the outer edge – OK

Step 8 – Add a ROUND on the intersecting edge that is near the curved surface with a radius of .06125.

Round Tool – value of .06125 – LMB the edge shown -OK

Step 9. Save the Clamp Ball part and move onto the next part.

Part 3 - Clamp Swivel

Step 1 – Create a Ne Part file a e Clamp_swivel .

Step 2 – Keep the U its i i h l se a d set the material as Steel.

File- Prepare- Model Properties- Material – change – double-click steel.mtl – OK - Close

Step 3 – Adjust the options so that 3 decimal places will be shown in sketcher.

File – Options – Sketcher – set the Number of decimal places for dimensions to 3 – OK- *No

Step 4-1 – Create a Revolve using the RIGHT datum as the sketch plane.

bottom and finish at the top of the arc, not the center of the arc. Using two lines in place of a single line

requires extra dimensions.

Tip: Start with the Arc first, as it is easier to have lines connect to the arc that vice versa!

Tip: Watch carefully for correct constraints and dimensions as this is a complex shape!

Step 4-3- Use the Normal Tool to create the shown dimensions*, noting that the arc is a Diameter

(double-click) and not a Radius (single-click) dimension.

Due to the complexity of this shape it may be required to have the dimension values set all at once using

Modify with regenerate turned off.

Modify Dimensions: LMB to drag a selection box across over all dimensions – select the Modify Tool – uncheck Regenerate – type in the values for the dimensions accordingly – press OK.

Step 4-4 – Accept the sketch and ensure the Revolve option is set to 360 degrees.

Step 5 – Rename and Set each Datum as shown below. RIGHT – Rename to B- Press Set - OK TOP – Rename to C- Press Set - OK FRONT – Rename to A- Press Set – OK

Step 6 – Use the HOLE Tool to create the first hole using the options below. Note that this hole will be drilled into a curved surface so a Datum must act as the primary reference plane instead of the curve.

Type: Simple, Diameter = .500, Depth = THRU ALL

Shape Tab Options: Set Side 2 to be THRU All

Placement: Linear Hole

Primary – Datum C - datum that runs the length of the middle of Revolve 1. Secondary

A) The flat end surface of the part (or Datum A). Set to a value of .5625 (or -.5625 if needed)

B) Datum B – The other datum that runs the length of the part. Set to Align or Offset of 0.00

Note – Hold Control while choosing the two Offset References.

Step 7 – Create a Round with a radius of .100 to the three circular edges as shown below.

Cosmetic Threads Step 8-1 - The shaft of the Clamp Swivel needs to be threaded. To save CPU power CREO can add a

Cosmetic Thread which tells the model that a thread of certain properties is present but will not show

up on the model graphic window.

Cosmetic Thread: Engineering drop-down arrow - select Cosmetic Thread to open the toolbar.

Step 8-2 – Select the Curved Surface of the Shaft as the Placement – select the Depth Tab – click on the flat annulus of the shaft end (the end of the surface to be threaded) to be the start surface – set the Depth to 4.00 and the Diameter to .4485.